Yep, a mounting hole in Kicad is basically just a footprint with a through hole pad on it. You put it on normal layers as any other component.

BTW, tip - if you add holes by hand (i.e. you don't have them in the schematics/netlist - probably nobody does), it helps to lock them in place so that they don't get removed when you reload/update your board from the schematics after any changes. That also prevents you from accidentally moving them around.

Yep, a mounting hole in Kicad is basically just a footprint with a through hole pad on it. You put it on normal layers as any other component.

There can be a bit more to it than that. Does the OP want the screw hole to be plated or unplated? Both are legitimate choices in different situations, and you can check what you've specified in the drill report file that KiCad can generate. For example, this board has both plated AND unplated 3mm holes:

I can't recall off hand how to specify the difference, but both are simple pads. I think maybe the unplated hole is made by having a pad size of zero, or maybe turning off the copper layers. Play around until the drill report file matches want you want.

Yep, a mounting hole in Kicad is basically just a footprint with a through hole pad on it. You put it on normal layers as any other component.

There can be a bit more to it than that. Does the OP want the screw hole to be plated or unplated? Both are legitimate choices in different situations, and you can check what you've specified in the drill report file that KiCad can generate. For example, this board has both plated AND unplated 3mm holes:

Sure, but that you can set when you are configuring the footprint/pad. Just set the pad type to "NPTH Mechanical" instead of the default and it will not be plated.

Well, I do... But locking the holes is a great idea in any case, to avoid accidentally moving them as you said.

Hmm, out of curiosity - how are you representing the holes in the schematics/netlist? Just put down any 1pin test pad somewhere in the corner? I can see wanting to do it if I wanted to make sure the holes are tied into the ground net, for ex, but not sure why I would do it otherwise.

Ah ha! I was trying to delete it but it won't delete references. Didn't think of hiding it.

Also, a tip to self... put the drill holes in for screws first. Means you stand a chance of laying the board out around them. In this case you can see I can't really use the other screw (top level User Drawing). I did try and move the DC jack around, but it looked like completely redoing the board to accomodate it.

Ah ha! I was trying to delete it but it won't delete references. Didn't think of hiding it.

Also, a tip to self... put the drill holes in for screws first. Means you stand a chance of laying the board out around them. In this case you can see I can't really use the other screw (top level User Drawing). I did try and move the DC jack around, but it looked like completely redoing the board to accomodate it.

One screw will do!

Jeeze, don't be lazy! It is not like you have hundreds of traces on that board, moreover the push & shove routing in Kicad will let you move things around with ease. Not putting a screw next to the power jack that will get unplugged and reinserted (thus loading the board mechanically) is a bad idea and you will likely pay for it by something getting broken over time.

Even regardless of the screws you should probably move the traces around the pin 8 of IC1 (hmm, any reason for using both IC? and U? conventions on the same board?) - that looks like asking for a short even though you have ton of space to move the trace above that pad. The traces between the pins of the P1 header the same story. Did this actually pass the DRC checks?

You have two layers, use them! It is better to put a via down and route the trace over the other side than to risk a short because of a trace too close to a pad. Murphy will ensure that you will get a stray piece of solder or a hairline short from the etching there and good luck finding that ...

If I move a component the tracks don't follow it. When I move the barrel jack down as far as I can I will still have the screw head screwing down onto the GND pad.

Besides, it's still a little draft as I'm not 100% certain on the footprint of the DC jack. It is assuming I go for a standard SMD one, but I think through hole might be cheaper. So when I make a concrete decision on that I'll try and move it to accomodate the screw.

I also have to test the size gain/loss with using a TO-92 version for U1 (LM78L05) as I already have them in stock (IC / U thing was just an oversight ) That will move things around a bit too.

I'm starting to realise that for these small boards you spend a lot of time starting from scratch, but each revision is 'usually' better.

It did pass DRC checks, but I think the nudge router is set to assume absolute minimum clearance is fine, maybe I should up my minimum clearance a bit until I need it lower.

However I already moved the tracks away from P8 on IC1. You are correct I should via down to the back layer for the pins on the other side of P1, thanks.

Besides, it's still a little draft as I'm not 100% certain on the footprint of the DC jack. It is assuming I go for a standard SMD one, but I think through hole might be cheaper. So when I make a concrete decision on that I'll try and move it to accomodate the screw.

If it is a regular barrel jack, I would probably go for a normal panel version - the kind that you make a hole in the enclosure wall and then fasten it with a nut and connect to the board using wires.

It did pass DRC checks, but I think the nudge router is set to assume absolute minimum clearance is fine, maybe I should up my minimum clearance a bit until I need it lower.

Check your design rules - normally the clearance should be set to about the same value as the track width, i.e. if I am using 10 mil traces, they should have at least 10 mil clearance too. Of course that's not an absolute rule but it is a good starting point.

If it is a regular barrel jack, I would probably go for a normal panel version - the kind that you make a hole in the enclosure wall and then fasten it with a nut and connect to the board using wires.

I'm actually struggling with the DC jack. The random SMD one I picked off RS Components for laying out the board that matched the default KiCad footprint is 10.5mm high, but it's 2.5mm pin diameter. I need 2.1mm.

Based on the drawings of the case (linked) I need something which is less than 11mm high (assuming a 1mm minimum board thickness).

In my experience the safest option is to order few of the jacks and measure them yourself. That's the only way to see how and whether it will fit - the dimensional drawings tend to be crap and often don't even match the actual part, especially when it is something generic like this. I have seen both Farnell & RS showing datasheets for a totally different component than what I was looking at, so beware!

The length shouldn't be a problem, IMO. If you don't have enough space on the board you can easily flip the voltage regulator or the microcontroller (or even both) to the other layer and move the capacitor (the advantage of SMD - they don't interfere with each other because there are no holes through the board!). Or use a flat tantalum type that doesn't take as much space. That will certainly free up quite a bit of space there. You can also gain space by moving the two pin header for the switch to the edge of the board - I am sure that one's position isn't critical because you are going to connect it using wires.

BTW, the best way to design things like this where you are constrained by the enclosure is to first position all the mechanical things that have to somehow interface with the box - screws, connectors, switches, etc and lock them down. If there are any protruding parts (e.g. a connector that will pass through the wall of the enclosure) don't forget to think about how the thing will be assembled - protruding parts on multiple sides of the board could prevent you from actually inserting the board into the enclosure!

Then place the remaining components because then you will see how much space you have to work with.

Personally I love this kind of work - it is a fun 2D-3D puzzle to work out and pretty satisfying when everything fits together. And also very infuriating when you assemble the board and discover that you have screwed up the position of something by a millimeter and it doesn't fit now.

I'm actually struggling with the DC jack. The random SMD one I picked off RS Components for laying out the board that matched the default KiCad footprint is 10.5mm high, but it's 2.5mm pin diameter. I need 2.1mm.

Usually this sort of jack comes in both flavors (2.1 mm and 2.5 mm). Same footprint, just different center pin size. I know Switchcraft parts are like that.

i have half a dozen DC jacks in the parts bin, but the PCB mount ones are 0.5A and not enough for the purpose. I have 2 panel mount ones and the ebay listing claims 3A... I'm suspicious though.

I might order a few different ones from RS and see whats what. I like the idea of the PCB mount as it will keep things neater and easier to just drop the PCB in and screw it in place without fighting with short link wires in a tiny enclosure, or making them long and spoiling the look of the semi transparent case.

Make sure you fix the footprint in your library! There's nothing like making the same mistake twice.

Yea, so as a final check I ignored everything except the traces on the screen and held the part up to the screen and ... even got my multimeter out and tested that the pins that go to 12V have continuity with the centre pin.

It wasn't that the footprint was mirrored it was that I had numbered the pins wrong.

It meant dropping the 12V under the ground on the back side, but that's what it's for.

I almost sent it with the silkscreen still saying GND on the 12V pin, but I think I would have caught onto that. Also nearly sent it without punching the ground onto the back plane with a few vias. Kicad DRC didn't catch that so it must see a ground connection somewhere, but I can't find it.

Anyway, fingers crossed. My first board is in the hands of EMS. This one is coming DHL, so it remains to be seen if I get stung for a customs handling fee... probably.